Maximum Workpiece Dimension: about 700mm x 60mm. Heigth depends on how you can fix the thing in there.

Cooling: Air (or liquids by hand

Clamping: Various - depends on your job

Runs via LinuxCNC (an Open Source CNC Software)

Standard Procedure

Warning Sign which is now implemented in the geilomat

There are some important steps to take, otherwise you can destroy everything - even the earth...
If you don't switch on the things in this particular order it can happen that the machine does things out of nowhere e.g. moves or turns on the spindle!!!

Check if the "Notaus" is physically triggered on the machine (Button is pressed)

Now power on the G4

Now plug in the FU ("Frequenzumformer")

Wait until the FU is booted

Check if 100.0 Hz is set on the screen of the FU

Otherwise rotate the rotary encoder that it is 100.0Hz

Now remove "Notaus" from the CNC

Power on the Machine inside LinuxCNC

Move near Homing position

Home the machine

Warm up the Spindle as described here in the wiki

Now the machine is ready to use.

For milling the spindle needs to be warm. The manual says that you should first let the spindle run for about 1 minute on 6000rpm, then increment by 6000rpm for 1 minute until you reached your destination speed. If the spindle wasn't used for longer than one week, you should double that time.
So better is to let it run for two minutes on each speed.

Parameters for typical jobs

Please note that these Values are produced under different circumstances - like how many "Schneiden" a mill has or what kind of mill you are using!
Please use also "Drehzahlrechner" for looking up proper values.

Material

Head Diameter mm

Cutting Depth mm (a_p)

Sidewards depth in % of diameter (a_e)

Spindle Speed

Feed Rate mm/min

Comment

MDF

8

2

?

12000

30

MDF is usually too thick to be milled with our normal milling heads, so we're using a bigger (8mm diameter) end mill. Plunge 10.

Wood

3

5

50%

12000-14000

>300

guessed proposal

Wood

0.8

4

100%

12000-14000

~250

guessed proposal

Aluminium

3

1

50%

6000

300

guessed proposal with cooling

Aluminium

10

10

20%

7990

3000

on an industrial machine, for comparison

Aluminium

6

0.25

6mm

10000

1100

Vierschneider, schleppender Schnitt - no external cooling

Aluminium

6

0.25

6mm

10000

650

Zweischneider, schleppend und ziehender schnitt - no external cooling

PCB engrave

0.1-0.3 30deg

0.3

12000

1000

tested in epoxy-pcb

PCB drill

0.9

-2.5

14000

400

tested in epoxy-pcb

Plexiglass Front door engrave

0.1 30deg?

1

10000

20

Plunge 20, toolsize cambam 0.3

Plexiglass egg

1.5 30deg?

0.5

14000

100

Plunge 30, toolsize cambam 1.5 : 4mm thick plexiglass 400x300

Plexiglas Portrait

0.1 30deg?

4

10000

?

0.3mm raster, Custom tool to convert from image to gcode

Warning:
Do not use a too low feed-rate!!
The cutting region of the milling head is microscopically round.
If the "Spanbreite", the thickness of the removed material, is lower that this radius,
most material is compressed and only cut if the compression force is to large.
This results in dramatic friction and hence only heats up the milling head.
The thought "Oh, the cutter is getting too hot, I can see burning marks in the side of the wood, I
have to reduce the movement speed" is deadly!!! You can decrease the spindle speed, and increase the movement speed.

The Heat produced while cutting depends on the friction. A second part is proportional to the volume of material that is removed.
Half the milling depth, half the heating! 25% sidewards instead of 50% sidewards cutting=half the heating.
Mill heads can break if the sidewards force is too large. So for tiny things,
the feed rate together with the spindle speed and the cutting depth should be reduced.

Pocketing plexiglass:

Choose engraving bit according to pocket size.

Be careful with CutIncrement (1mm is ok).

Be aware that plexiglass melts, so it's important to use cooling.

For bigger pocket operations, the vacuum cleaner has a certain cooling effect.

Air pressure and water cooling was necessary for the front door window engraving.

Technical Foobar

Current Status

Max-Movement speed is approx 2000 mm/min.

Homeing procedure in EMC is functional, and by that also soft-limits. Its now "nearly" impossible to move over some limits. Start EMC, turn machine on with f1/f2, press "home all", wait 30 sec. Than traverse to the wished zero of your working coordinate system, and touch off in all three axes.

The Spindle, aka the Mechatron, is switched on/off automatically.

Spindle speed must be set to a value between 6000 and 24000. Use GCode like M3 S6000

The Spindle needs some warmup before running. Manual says One minute on 6000rpm, then increase in steps of 6000 until the whished speed is reached. stay for one minute on each level. If the spindle is very cold and has not run about a week double the times!

technical details

A CNC mill like the dear Geil-O-Mat has three axis that can be moved independently. A spindle with a mill cutter typically removes material.

Some pink work in progress...

Each axis is driven by one (Y and Z) or two (X) stepper motors. Basically, theses motors can only rotate in 1.8 degree steps, and hence no secondary encoder is needed for the machine knowing its current location. By a trick called "microstepping", currently the resolution is increased to 1/8 of 1.8 degrees.
As the stepper leads in to a "Zwillings-Trapezgewindespindel", the rotation is transformed into linear motion, one revolution= 6mm.
Warning: If there is too much force for the motor to move one step, it skips the step, typically failing also in subsequent movements, resulting in an ugly noise, and shift in the positioning.

The motors are connected to a driver device, which sits on top of the whole machine. It creates the strong currents for the stepper drivers, out of signals from the PCs parallel port.

Hence, the computer has to send signals telling which axis should move one step forward or backward at a given instance. This can/is done by a software called "EMC". It is open source, and the thread doing this parallel port communications is using the patched real time Linux-kernel.

There are some GUIs for EMC, the most relevant is "AXIS", which graphically displays the current machine position, the paths it should travel the track history, and further stuff. Also manual movement can be performed.

The language to specify the movement of the machine is called "GCODE". Some of its statements are starting with G01,or G00, hence the name.
A simple Gcode can look like this:

; i am a comment
F100; move with 100mm/min while cutting
G0 Z10; fast move to Z-coordinate 10
G1 Z0; drill down until Z=0 with the speed given by the Feedrate
G1 X10; move to the new location X10 while cutting
G0 Z10; and back up with large speed.
M30; end program

One can do a lot of things, e.g. have variables (#1=10), and do loops , evaluate mathematical expressions (G1 Z[#1*2] ).
So basically, real hackers write gcode by hand, while Chuck Norris sends movement commands to the steppers.
However, as we are all lacy, and things can get quite complicated, there exists software to convert 3d/2d CAD files, grayscale depthmap images, 3d-stl objects and other things into Gode. This is often called "CAM"-Software.

If you have a 2d-cad file (e.g. dxf) and specify depths for some areas that should be milled away, one speaks of 2.5D-CAM. This is performed e.g. by CamBam, or Camexpert.

The biggest trouble is the radius compensation of the milling heads. You always have to cut on a path half a diameter outside of the actual position. For this, there are various workflows. In Gcode, one can tell specify if one wants to cut left, right or directly on the actual path. This is called cutter radius compensations. Its a pain in the ass. Hence, often one uses no such thing, but either draws directly the offsetted lines in CAD, or has some software like cambam, which does this compensation and outputs already compensated "paths". The drawback of both methods is that one can not change the diameter of the cutter without recreating the gcode.

In the Gcode compensation, a "tool table" is used. Each cutter is index by a number, and in the table the diameters and other things are specified.

The current machine's state is given by a coordinate triple, and some states (emergency swich, spindle speed, ...). The machine coordinate system is defined by the now automated homing routine. Thereafter, one can move the machine to a location, and "touch off", giving explicit coordinates for this location. Thereby the working coordinate system is defined. This is also the system displayed in Axis, However, in the background, the machine still works in the home-coordinate system for checking its movement limits. Clever!

CNC PC

On the CNC PC runs a Ubuntu version with a realtime kernel and 2.6 LinuxCNC. Because the dependecies for linuxcnc are really messed up, please do not try to update the PC! --Reox 14:36, 31. Aug. 2013 (CEST)

The PC has a Backup Harddisk, which contains a complete working system image for system restore.

The linuxcnc config folder (/home/cnc/linuxcnc/config) is a git repo, so please commit your changes if you changed something on the config.

Better: If you want to try new settings copy the Geilomat config and create your own - the Geilomat setup should be sufficant for everyone, so you need good reason to change it

The PC has APIC disabled, because of realtime kernel jitter reasons. so if you power it down, you need to press the power button after the system says "system halted"